Stats

  • Locked Locked
  • Replies 4
  • Subscribers 164
  • Views 14247
  • Members are here 0
More Content
This discussion has been locked.
You can no longer post new replies to this discussion. If you have a question you can start a new discussion

Pads to Allegro Conversion Problem

archive

Hi Folks, We recently migrated to Allegro ver 16 from Pads layout 2005 spac2,we could able to convert the Pads pcb design file to Allegro,the pcb file is 4 layer,later we extracted all the footprints in separate folder and set the path in the user preferences. Now while i try to compile the schematic alone in which i had entered the footprints details extracted from allegro,i don't encounter any problem as such,but then while i try to compile it to the Allegro database,it doesn't convert to Allegro environment it encounters 78 errors,it goes like this... #1 ERROR(SPMHNI-191):Device/Symbol check error detected. WARNING(SPMHNI-337)Unable to load symbol "TP100X40" for device 'TP_1_TP100X40_485_A': WARNING(SPMHNI-127):Could not find PADSTACK PAD21. due to ERROR(SPMHDB-274):Unable to load flash symbol PAD21(Check PSMPATH setting for this symbol) Error is similar for all the 78... Since iam novice to Allegro,i tried edit the footprints individually,for every smd components,it refers some flash pad in the thermal layer>padstack layer and i was asked by the application engineer to delete and update, but still i encounter same problem. Later i was asked to edit individual Pads used in the library from Pad designer,i observed the flash Pad still existing in the thermal layer,i really dunno how to take it from here..... Is this flash pad in the thermal layer>padstack layer causing the problem? If someone could help me out from this mess would be greatly appreciable. Thanks & Best Regards, Ramesh


Originally posted in cdnusers.org by rame
  • archive

    Here's what I do when converting PADS designs.

    1) translate the database
    2) open all the symbols ; modify accordingly
    3) Modify the padstacks inside the symbols; correct them; save them; refresh the new padstacks into the symbols.

    When you mod the padstacks, you'll find extra things (flash descriptions, missing soldermask definition, etc.) Clean them, refresh them, and save them with a "good" padstack name. :)

    You should be good to go then.

    Good day.
    Mitch


    Originally posted in cdnusers.org by cadpro2k
  • archive

    Hi Mitch,

    Thanks for the reply,i did followed the step you have mentioned before posting my query here in this forum,

    1) I converted the 4 layer pcb from Pads to Allegro.

    2) Extracted all the footprints to separate library.

    3) opened each dra file and edited the extra flash thing and updated.

    After this three steps i could able to compile the orcad cis schematic alone,but then while i try convert it to the Allegro database,above said error appears,please look my first query for details.

    Later i was asked to edit each pads in the Pad designer(like Pad1,Pad2 etc) which has been used by the dra file(lib),but then i observe edited flashes which i edited earlier for each dra(symbols) reappears again.

    am i missing some step along...


    Thanks & Best Regards,

    Ramesh


    Originally posted in cdnusers.org by rame
  • archive

    Later i was asked to edit each pads in the Pad designer(like Pad1,Pad2 etc) which has been used by the dra file(lib),but then i observe edited flashes which i edited earlier for each dra(symbols) reappears again.



    When updating the symbols, here's what I do:
    1) open the symbols
    2) edit the padstacks
    - remove flash descriptions
    - add the soldermask
    - add the paste mask definition
    - "save as" a new padstack name (in your central library)
    - refresh the local symbol padstack with these NEW padstacks from your central library
    3) check you have NO remaining "converted" padstacks in your symbol (refresh_padstacks)
    4) save the symbol

    This makes sure your parts are accessing "approved, good" padstacks.

    You shouldn't then have a problem (Always be aware if you have multiple locations for reading padstacks and symbols (e.g local vs. central libraries)

    Good day.
    Mitch


    Originally posted in cdnusers.org by cadpro2k
  • archive

    Hi Mitch,

    Thanks for your reply,i followed the steps mentioned in your previous mail and could able to fix the issue,thanks
    a lot.

    Thanks & Best Regards,

    Ramesh


    Originally posted in cdnusers.org by rame
Cadence Guidelines

Community Guidelines

The Cadence Design Communities support Cadence users and technologists interacting to exchange ideas, news, technical information, and best practices to solve problems and get the most from Cadence technology. The community is open to everyone, and to provide the most value, we require participants to follow our Community Guidelines that facilitate a quality exchange of ideas and information. By accessing, contributing, using or downloading any materials from the site, you agree to be bound by the full Community Guidelines.